error in Analysis

[Asad005]

Dear, I am receiving the following error when I run the 3D model. Can plz help me out in indicating the issue?

Error: Fracture energy (Gf = 0) is too small, or the element characteristic length (lch = 11.727) is too large.
The maximum allowed lch is 2*E*Gf/(s0^2) = 0 with:
E = 28750
Gf = 0
s0 = 1.32

In function: void __cdecl DamageLaws::ExponentialSoftening::compute(double,double,double,double,double,double &,double &)
In file: C:\Develop\OpenSees-plugins\src\damage_laws\ExponentialSoftening.h (Line: 28)
Press any key to continue . . .

[STKO Team]

It says what it says... Gt = 0 is too small (in fact it is 0). Make it larger

[Asad005]

Thanks,
I did it.
Do I need to restraint my 3D model in out of plane direction if I am applying loads only in in-plane directions?
But please can check these two errors which I received after RUNNING THE analysis. I think there is some error with constraints of the 3D in the first case.
1.
WARNING PenaltySP_FE::setID(void) - unknown DOF 3 at Node
WARNING PenaltySP_FE::setID(void) - unknown DOF 4 at Node
WARNING PenaltySP_FE::setID(void) - unknown DOF 5 at Node
WARNING PenaltySP_FE::setID(void) - unknown DOF 3 at Node
WARNING PenaltySP_FE::setID(void) - unknown DOF 4 at Node
WARNING PenaltySP_FE::setID(void) - unknown DOF 5 at Node
WARNING PenaltySP_FE::getTangForce() - constrained DOF 3 outside disp
WARNING PenaltySP_FE::getTangForce() - constrained DOF 4 outside disp
WARNING PenaltySP_FE::getTangForce() - constrained DOF 5 outside disp

2.
Increment: 1. time_increment = 0.1. Current time = 0.0
WARNING MumpsParallelSolver::solve(void)- Error WARNING MumpsParallelSolver::solve(void)- Error WARNING MumpsParallelSolver::solve(void)- Error -13 returned in substitution dmumps()
out of memory wanted 1429064906 (if < 0 mult absolute by 1 million)
WARNING ModifiedNewton::solveCurrentStep() -the LinearSysOfEqn failed in solve()
StaticAnalysis::analyze() - the Algorithm failed at iteration: 0 with domain at load factor 0.1
-13 returned in substitution dmumps()
out of memory wanted 1429064906 (if < 0 mult absolute by 1 million)
WARNING ModifiedNewton::solveCurrentStep() -the LinearSysOfEqn failed in solve()
StaticAnalysis::analyze() - the Algorithm failed at iteration: 0 with domain at load factor 0.1
-13 returned in substitution dmumps()
out of memory wanted 1429064906 (if < 0 mult absolute by 1 million)
WARNING ModifiedNewton::solveCurrentStep() -the LinearSysOfEqn failed in solve()
StaticAnalysis::analyze() - the Algorithm failed at iteration: 0 with domain at load factor 0.1
OpenSees > analyze failed, returned: -3 error flag
ERROR: the analysis did not converge
while executing
"error "ERROR: the analysis did not converge""
("for" body line 23)
invoked from within
"for {set increment_counter 1} {$increment_counter <= $initial_num_incr} {incr increment_counter} {
if {$process_id == 0} {
puts "Increment: $increm..."
(file "analysis_steps.tcl" line 7398)

[STKO Team]

It looks like you defined a 2D model, but then you are trying to constrain DOFs such as Uz Rx Ry which are not available in a 2D model

[Asad005]

Thanks for your response.
I removed the restraints last day but still have an error in analysis.
And also change the load at the tip of the beam to the displacement and from beam to the bar with the rigid link in constraints.

Can you please have a look of the model, I am going to attach herewith?

[STKO Team]

Dear Asad,

Here is a working version of your model:

REalfon 3D, PAssign, merged.zip

(856.83 KiB) Downloaded 207 times

There are many issues in old your model. I will try to summarize them here.

• you merged solids (column and beam) with the edges of the rebars, however that boolean operation is not valid, because the edges for the rebars do not intersect with the solid boundaries (they are embedded). The best solution would be to cut the solid at the same location of each rebar, but it takes time. So I used an EDOF between solid and rebars, using a mesh seed that more or less makes the mesh of the rebars and of the solid, almost equal.
• I changed some conditions that were not working as expected.
• The top constraint fixes the Z disp, but in this way the the vertical load is not applied. So I un-fixed the Z disp, and added it later on after the vertical analysis
• the vertical analysis should be done before applying the horizontal load
• I used a DamageTC3D also where you used an elastic material. Of course using material parameters such that it will always remain elastic. This is not mandatory, but we noticed that there is a bug in the output of the ElasticMaterial if you ask for Damage.

[Asad005]

More than thanks for your help

[Asad005]

Request for one more question.

How you meshed the entire model regularly. As I am trying to regularize the mesh but not working especially for the brick element.
So can you please let me know how to find the mesh size for a regular mesh of a model?
The mesh doesn't coincide with that of the element assigned (brickSSP) and unable to get square regularly meshed model.
Sometime meshing up to very small size, the STKo get closed directly and then I have to reopen it again from the start to mesh the model.

[STKO Team]

Looking at the error, it looks like you assigned a Brick element (which is an Hexahedron, that expects 8 nodes) to a geometry meshed with 3-node elements. probably because you assigned it to a surface (rather then a solid), and that surface is meshed with triangles.

Furthermore, In order to mesh a solid geometry with a regular structured hexa mesh, the model should be made of 6-faces (prism-like) solids, attached together with a merge command.